Drill peck with a dwell?

So I’m going to be upgrading my waste board to aluminum. I’m planning to spot drill the hole layout with the CNC. I would like to have a dwell at the bottom of the spot, to ensure depth accuracy. I’m using v carve pro, with both gcs and easle. The program file doesn’t seem to have a dwell in it, even though I’ve checked the dwell box in v carve. Any thoughts?

Can you share the gcode?

Here’s the beginning of the file. I’ve run it as a test, with a 1, 2, and 3 sec dwell and it has no noticeable effect while running and no difference I can see in the program file.

T1
G17
G20
G0Z1.0000
G0X0.0000Y0.0000S16000M3
G0X0.5000Y0.5000Z0.0600
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X1.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X2.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X3.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X4.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X5.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X6.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X7.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X8.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X9.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X10.5000
G0Z0.0200
G1Z-0.0950F5.0
G0Z0.0600
G0X11.5000
G0Z0.0200

I know on my machines at work, (i’m a machinist), a dwell is a G4. Not sure if it’s the same for grbl. I would assume so.

No G4 commands in the G-code. How did you generate the G-code? What program? What did you do to try to generate a dwell?

1 Like

Same command in grbl.

I used V Carve pro to post out the g code. The tool is a drill peck cycle. There is a check box for dwell at the bottom of each peck cycle/bottom of the hole. It’s checked, and I’ve adjusted it and reposted with 3 different intervals. no go.

What post processor are you using?

I’m assuming you mean how I’m saving the file? I have the X Carve (in) selected.

Do you know how to add post processors?
Go to File–>Open Application Data Folder…
Open the PostP folder, and add this file:
X-Carve_inch_DWELL.pp (4.4 KB)

Use that one when you save your gcode.
You may have to restart V-Carve for it to show up in the list.

Here are some others for anyone else, modified to include the G4 dwell: (GRBL ones will overwrite existing…didn’t see a reason to not have the ability. X-Carve versions will not overwrite your current ones.)

X-Carve_mm_DWELL.pp (4.4 KB)
Grbl_inch.pp (4.5 KB)
Grbl_mm.pp (4.5 KB)

A bit too much celebrating for the 4th, and I find myself reading a manual on Vectric Post Processors. :crazy_face: Have yet to use V-carve for a project.

2 Likes

Thanks for the help! Haha. I’ll give it a try later today. Still waiting for my aluminum to get delivered. It may be today. Crossing fingers!

Yay! it worked in the code. I’ll run a test just to verify. But Thanks for the help! It would have sucked hand editing the file. There’s a ton of lines that would have had to have been inserted.

T1
G17
G20
G0Z1.0000
G0X0.0000Y0.0000S16000M3
G0X0.5000Y0.5000Z0.0600
G0Z0.0200
G1Z-0.0950F5.0
G04 P1.00
G0Z0.0600
G0X1.5000
G0Z0.0200
G1Z-0.0950F5.0
G04 P1.00
G0Z0.0600
G0X2.5000
G0Z0.0200
G1Z-0.0950F5.0
G04 P1.00
G0Z0.0600
G0X3.5000
G0Z0.0200
G1Z-0.0950F5.0
G04 P1.00

1 Like

Glad it worked out! Make sure you share your wasteboard upgrade.
For anyone else: The most current version of the Vectric post processors do not include support for a dwell. The files shared above add that support.

1 Like

No. I’ve only looked at the ones I just installed. I’d guess they never included it.

1 Like

Any reason not to spiral down with an endmill? The gantry may not appreciate the vertical forces.

1 Like

I think @Phantomm is suggesting using, for example, a .125" end mill to create a .25" hole.

1 Like

Yupp. Forgot the term. :sweat_smile:

1 Like

I have completely switched to the helical bore with ramping. Works like a champ.

Well, I’m more concerned about time. That would definitely take longer. Just finished spotting all 961 holes… Took about 1.5 hrs. I went a little on the conservative side, plus a dwell of 2 sec. I haven’t received my cnc4newbie z axis yet.

2 Likes

The base holes don’t really matter unless your using pins to align stock. And then it’s useless unless you were super careful to square the machine before the op.
Either way it’s looking really nice and that tone you hear is jealousy. :stuck_out_tongue_winking_eye:

2 Likes